Perform a basic model check, as outlined in [24]. For example, you can use LS-PrePost (Application > Model Checking > General Checking > Keyword Check).

Inspect the model carefully with respect to element quality, small (or even negative) initial volume of solid elements, and small Jacobian values.

To some extent, the explicit time step listing in the d3hsp file can be used as an element quality indicator. For example, if the first listed element has an explicit time step which is several orders of magnitude lower than the others, it can be an indication that this is maybe an element which violates the quality criteria. The following figure shows an example of a time step that might indicate a problem with an element. Element number 864683 (highlighted in the following figure) has a time step that is about 1000 times smaller than the other elements. This indicates poor element quality.

Figure 11.6: Example of listings of explicit time steps in the d3hsp file

Check the model connectivity. Unconnected sub-assemblies or "loose parts" cause rigid body modes in implicit statics, potentially causing convergence problems. One indication of this problem is negative eigenvalue warnings like the following in the d3hsp file.

 *** Warning 60124 (IMP+124)
 XX negative eigenvalues detected

Unintentionally loose sub-assemblies that start to spin can cause slow convergence in implicit dynamics. Ways of checking model connectivity are:

In many analyses, the presence of rigid body modes is intentional. A typical example of this is an assembly that is to be connected via bolts and contacts. Before the bolt pretension is applied, such an assembly has many rigid body modes [22]. Set IMASS = 1 on *CONTROL_IMPLICIT_DYNAMICS to activate implicit dynamics, at least during the initial phase, until contacts are fully established. This normally solves convergence problems due to intentional rigid body modes (see Bolt Pretensioning). In some cases, inertia relief boundary conditions (applied by *CONTROL_IMPLICIT_INERTIA_RELIEF) are relevant for handling intentional rigid body modes. In cases where the rigid body modes are unintentional, due to forgotten boundary conditions, for example, simply apply the appropriate boundary conditions.

Verify that the element connectivity is valid. Be cautious when continuum elements (typically solids) and structural elements (beams, shells) share nodes. Invalid connectivity can cause unintended hinges, joints, or other mechanisms. For example, connecting a beam element between two solids using only shared nodes leaves the possibility for the beam to spin freely around its axis. Connecting shells to solids along a single row of nodes could create a hinge. In some cases, the program issues warning messages for potentially problematic connectivity, for example:

 *** Warning 60301 (IMP+301)
            Using *CONSTRAINED_SPOTWELD with nodes without rotational dofs.

Avoid the use of release conditions on constrained nodal rigid bodies (CNRBs). It is not recommended to use DRFLAG,RRFLAG ≠ 0 on CNRBs (other than for two-noded CNRBs in linear implicit analyses, NSOLVR = ±1 on *CONTROL_IMPLICIT_SOLUTION). If release of degrees of freedom is required, use joints (*CONSTRAINED_JOINT_...) instead.

From R11 of LS-DYNA, joint stiffness and damping can be applied globally on *CONTROL_RIGID by the variables GJADSTF,GJADVSC, TJADST and TJADVSC. This allows for the addition of a small artificial stiffness to improve convergence of models with numerous joint definitions.

As a troubleshooting step, disable joint failure (switch *CONSTRAINED_JOINT_{TYPE}_FAILURE to *CONSTRAINED_JOINT_{TYPE}) at least in the initial model development phase.

Check tied contacts. This is often closely related to the model connectivity since tied contacts are often used for assembling different parts or sub-assemblies of a model.

Using a tracked node set gives better control over the possible tied nodes than if a tracked part set is used. The tie distance can be manually adjusted as described in Tied Contacts. When using constraint-based tied contact, nodes subjected to other constraints (*CONSTRAINED_NODAL_RIGID_BODY, *BOUNDARY_SPC, ...) cannot be tied. One remedy may be to set IPBACK > 0 on Optional Card E of the *CONTACT_TIED_ definition. The program automatically creates a penalty-based tied contact for nodes that are subjected to other constraints.

Avoid unintended initial penetrations in contacts. The IGNORE = 2 option of Mortar contacts can handle "reasonably large" initial penetrations, but a penetration free initial configuration is always preferred.

Most preprocessors have built-in tools for checking and correcting initial penetrations, for example LS-PrePost accessed via Application > Model Checking > General Checking > Contact Check > Penet.

Mortar contacts report initial penetrations in the mes0* files. Look for:

 Mortar contact information for contact ID …

This information can be used to verify that the contact penetration checks of the preprocessors agree with how LS-DYNA interprets the initial contact state.

Initial penetrations may be reported in the d3hsp or mes0* files but not be found in the preprocessor (refer to the figure below for an example). To fix this, specify a reasonably small "contact thickness" for solids using the PENMAX parameter (compare Figure 6.1: Using PENMAX to define the contact thickness for solid parts.).

Figure 11.7: Example of spurious penetration detected by the Mortar contact

The left side of the image above shows an extract from the d3hsp file where the elements are reported as penetrating, even though they are clearly separated, as shown in the illustration on the right.

From R12 of LS-DYNA, penetration information can also be visualized (fringe plotted) from the d3plot file by setting PENOUT = 1 or 2 on *CONTROL_OUTPUT.

When you know beforehand that no self-contact within the same part occurs and a single surface Mortar contact is used for convenience, the option IGNORE = -2 can improve convergence by neglecting self-contact within the same part, avoiding spurious self-contact.

Use IGNORE = 3 or 4 of the Mortar contact [23] to resolve press-fits or other intended initial penetrations.

When shell parts with varying thickness are involved in Mortar contacts, it is often beneficial for convergence to define the thickness variation by *ELEMENT_SHELL_THICKNESS rather than splitting up a (physical) part into many different parts with the thickness variation defined by different *SECTION_SHELL.

For 2D analyses, use the appropriate 2D contacts, see Contacts for 2D Analyses.

Check the material models.

Figure 11.8: Example of hardening curves - avoid a negative slope for the last segment (dashed red line)

The d3iter file provides useful visual information that indicates reasons for the convergence problems. For example, looking at the deformation of a non-converged state shows whether loose parts "fly away" due to rigid body modes.

Is the physical problem itself unstable? Does collapse, buckling, or bifurcation occur? If the applied loading exceeds the ultimate capacity of a structure, convergence in implicit statics is, in practice, impossible to reach.

For analyses involving rubber (or other incompressible materials), try disregarding the initial geometric stiffness effect by setting IGS = 2 on *CONTROL_IMPLICIT_GENERAL.

Switching to a full Newton solution scheme can be efficient for solving highly nonlinear problems. This means that the stiffness matrix is reformulated and factorized for each iteration.

Activating the non-symmetrical equation solver can improve convergence in some cases, for example follower loads, "snap-through" deformation, or contacts with high (µ ≈ 0.3 or above) friction. It can also prove convergence for cases involving anisotropic material models.

Set LCPACK = 3 on *CONTROL_IMPLICIT_SOLVER.

Check for "too easy" convergence. This means that LS-DYNA has previously accepted a state even though it was not converged "enough" (that is, some residual forces or deformations remain in parts of the model). When proceeding from this state, the residuals might lead to non-convergence, since the problems from previous steps remain unresolved.

Some clues may be found by tracking the convergence information regarding the line search history, see Figure 11.1: Tracking convergence information in the mes0* files. Typically, the line search should converge within 10 iterations. If the line search requires significantly more than 10 iterations to converge and the residuals remain high even with very small step sizes, nonconvergence may be due to severe overloading of the structure. In such cases, check that consistent units are used and the loading has the correct order of magnitude. If the loading is correct, it might help to reduce the time-step size.

Note that the node ID/rigid body ID with the maximum residuals are listed in the iteration information (see Figure 11.1: Tracking convergence information in the mes0* files). Inspecting the model at these ID:s and perhaps, their surroundings might provide insight about what is causing the convergence problems. This can be, for example, poor element quality or unconnected parts. This is especially likely if the same ID:s show up as critical for several consecutive iterations. These entities can be highlighted on the model using the D3hsp View tool, see Figure 11.5: The D3hsp view-tool in LS-PrePost and by tracking the convergence histories, as shown below.

Figure 11.9: Tracking the convergence histories using the D3hsp View tool in LS-PrePost

For extended interactive troubleshooting, you can send sense switch controls to the Ansys LS-DYNA software. Create a text file named d3kil in the directory where the current simulation is running. The text file should contain one of the following text strings to control the implicit analysis:

For more information on using sense switch controls, see the Getting Started section of Keyword Manual Vol. I.

Converting the model for explicit analysis (see Converting an Implicit Model for Explicit Analyses for details) can give valuable insight for troubleshooting (such as unconnected parts "flying away").

In cases when convergence cannot be obtained using the implicit solver, switching to explicit analysis is an alternative option for obtaining a solution.

Residual histories, iterations to converge, etc. may also be plotted in LS-PrePost (starting at version 4.5) using Misc>D3hsp View, see Figure 11.9: Tracking the convergence histories using the D3hsp View tool in LS-PrePost.